It works on mine. I did a 2" translate, 4 copies, to the right and it posted:
G54
G55
G56
G57
I saved it and reposted it here. See if it doesn't work now.
Greg
Maybe it will make you feel good to know that because of this thread when we met with the MasterCam guy recently I was able to ask questions that made it appear I knew far more than I really do about the multiple work zero output. I also was able to ask questions about things like trochoidal machining and face peeling.
So you guys should feel thoroughly brain-picked.
When we placed the order he asked my Production Manager how many MasterCam Tee-Shirts we wanted. The answer was that if we didn't want to play favorites it had to be none or sixteen so we could give one to each guy; so now we have sixteen $1,000 tee-shirts and they threw in two MasterCam seats as an extra.
P.S. Haas Apps you owe me about 1200 Haas Tee-Shirts.
An open mind is a virtue...so long as all the common sense has not leaked out.
That's good news, Geof. If I read enough of your posts, I might someday take "CNC nOOb" off of my signature line.
Greg
Should I post a picture of me in a MasterCam Tee-shirt?
An open mind is a virtue...so long as all the common sense has not leaked out.
Toby D.
"Imagination and Memory are but one thing, but for divers considerations have divers names"
Schwarzwald
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
www.refractotech.com
Yup, standard Haas post. What version of Mastercam are you running? I've made some minor tweaks to my post so I'm not sure if I'd be comfortable recommending it (I don't remember what I did--it's been awhile).
You opened the file and didn't change anything, right? Are you SURE that it didn't create the extra work offsets? I'm assuming that you searched for G54 and found it multiple times. That's correct since it's going to do one operation at G54, then G55, G56, G57, then start over with the next op: G54, 55, 56, etc.
Did you also search for G55, G56, etc?
Greg
Yup, I found no G54, G55, etc in the posted file at all. I have also made some changes to my post I don't remember (trying to learn things and all), let me see if I can find my original unmodified machine definition and post and try posting with that.
Thanks so much for helping!
-Taylor
Hey sorry I haven't been back here, work has been busy and all.
So I'll have to keep looking, I don't think I was able to locate my unmodified post so I'm not sure if my issue is the post or not. Do you mind sending me your post just so I can verify it's not something else? I know you said you don't recommend using it, I just want to make sure my post is the issue.
Thanks,
-Taylor
You can send it to my email at tlalexander <ignore this part> ~at~ gmail "dot" com
facegarden, what version of Mastercam X are you running as this makes a difference on the post. I wanted to share but need exact version or the post wont work.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Cadcam
Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .
I just have X1.
-Taylor
So, it seems I can't get anything to post with multiple work coordinate systems.
I've tried just making two drill points and setting each one to its own WCS, but when i post, it still just acts like I had set them both in the same WCS.
Is that more likely in my post, or in my machine or control definitions?
Attached is what I have under the "work system" tab in my control definitions, if that makes a difference.
Thanks,
-Taylor
Did you get my email? I sent you the post. Have you tried it?
Greg
Ah! Sorry, i get so many e-mails that sometimes I miss things!
Well turns out your post works!
Furthermore, I was able to get my post to do it!
We have slightly different functions for
"pwcs #G54+ coordinate setting at toolchange"
Yours is:
Mine was:Code:pwcs #G54+ coordinate setting at toolchange sav_frc_wcs = force_wcs if sub_level$, force_wcs = zero if workofs$ <> prv_workofs$ | (force_wcs & toolchng), [ if workofs$ = -1,workofs$ = 0 if workofs$ < 19, g_wcs = workofs$ + 54 else, g_wcs = workofs$ if (workofs$ > 5) & (workofs$ < 19), g_wcs = g_wcs + 50 if (g_wcs < 54) | ((g_wcs > 59) & (g_wcs < 110)) | (g_wcs > 122), pwcs_bad else, g_wcs ] force_wcs = sav_frc_wcs !workofs$
I noticed mine had the "if mi1$ > one" condition. The rest of my WCS code seemed to be sensible, but yours didn't have that if statement. I wondered if my post was failing that IF condition and never setting the WCS, so i removed the if statement and everything works!Code:pwcs #G54+ coordinate setting at toolchange if mi1$ > one, [ sav_frc_wcs = force_wcs if sub_level$, force_wcs = zero if workofs$ <> prv_workofs$ | (force_wcs & toolchng), [ if workofs$ < 6, [ g_wcs = workofs$ + 54 ] else, [ g_wcs = workofs$ + 104 ] if workofs$ >= 0 & workofs$ <= 25, *g_wcs else, [ if mprint(swcserror, 2) = 2, exitpost$ ] ] force_wcs = sav_frc_wcs !workofs$ ]
I have no idea what that will do to other things, I am going to need to start looking into what all this stuff in the post means, but for the record and in case it wasn't clear, I ended up with that section of my post like so:
The only real thing I noticed is that mine only allows 6 consecutive WCS's above G54 while yours allows 19, which my machine wouldn't support, I don't think.Code:pwcs #G54+ coordinate setting at toolchange sav_frc_wcs = force_wcs if sub_level$, force_wcs = zero if workofs$ <> prv_workofs$ | (force_wcs & toolchng), [ if workofs$ < 6, [ g_wcs = workofs$ + 54 ] else, [ g_wcs = workofs$ + 104 ] if workofs$ >= 0 & workofs$ <= 25, *g_wcs else, [ if mprint(swcserror, 2) = 2, exitpost$ ] ] force_wcs = sav_frc_wcs !workofs$
Anyway, anyone know what I deleted?
Thanks!
-Taylor
Donkey Hotey,
Thanks for your posting on 10-25-2008, 10:41 PM. This was exactly what I was looking for. Your old posting really helped me.
Again, THANKS!
Mike